What is the best way to test a spreader beam?

For a little while now I have been experimenting with running studies on the capabilities of a design of spreader beam that I have come up with. The only issue is I am experiencing difficulty with being able to constrain/define the "chains". At first I thought of modelling them as truss elements as axial loading was all that I was concerned about on the chains but I could not bond the end of the truss to the face of the shackle. The scope of my study is to see the maximum stress and displacement on the beams. The chain I have had to model crudely because I feel its impact would help to aid a more realistic approach to crushing the beam as it would in reality.

I am somewhat stuck at the moment, and any help would be greatly appreciated. I have ran some hand calcs on this and I know it can withstand the load but I would still like to simulate this in SOLIDWORKS. I have attached my model for reference.

The load is perfectly vertical on the bottom hole and the chains can flex but the top face I have attempted to fix with a 0 translation reference geometry fixture in all directions. I still wish it to rotate if necessary. Also I havent been getting symmetrical results which is concerning.

If the assumptions you make are correct then you're able to simplify the simulation and the time(money) spent on it. So why not?

You've probably already spec'd out the chain and shackle which have been tested and should have a certified load rating for lifting so they're more than likely not the point of concern.

I created a split line on the face of the holes and applied a Fixed Hinge fixity to the divided face. It looks like there are stress concentrations around the split line and I haven't tested the mesh to see if it converges. You could treat the tube as beam elements for a faster simulation.

I'm not sure if this is the right way to do something like this but it did work.

Attachments

The "best way" to simulate a thing is always to be stubbornly accurate and literal.

I model chains often. Usually a link connector works, but an extension-only spring is better, if there's a chance of it losing tension. A single vertex with take the load on each end, so there will always be a stress concentration to account for. One must also make the vertex - here I used a surface split. I set this up with link connectors running to a simple fixed block.

The non-zero size of the block provides some stability to the system. Refining the block keeps a couple elements between connectors and fixtures.

Normally I would use pin connectors for the shackles, but pin connectors are broken in SW 2018 and 2019 (so far). High-accuracy no-penetration contact is the most general and accurate way to do pretty much anything in Solidworks Sim.

Attachments

Thank you Shawn for your very detailed reply! I am very grateful. I cannot see your attachment however?

Your reply makes a lot of sense, the stress concentrations I will ignore as the chain and the shackle I know are more than capable of taking the load. I just wanted to see what effect it would have on the beam.

Thanks once again for your efforts, I look forward to seeing your model.

Wow, that's rather impressive. I've done this many times before and I almost never add hardware (purchased component - sized appropriately). Sometimes I do add a physical 'pin' just to get a better force transfer and use contact surfaces.

A link is supposed to be a rigid point-to-point connection, enforcing a distance between two points. There is no resistance to lateral (off-axis) movement. So if a chain is for sure always in tension, and does not stretch a meaningful amount, then the link connector serves well.

Again an extension-only spring is technically more appropriate, if there's a chance of the chain going slack or if you want to include linear stretch under load.

The right way to apply these loads is with a 'bearing' force, which distributes the force over only the proper half of the cylindrical face. I hardly use them because it requires making a 3D sketch to locate and orient a new coordinate system for every load. It's faster (in human time) to grab an existing part, or even model a simple body, to input the load through a contact set.

In many cases the detail won't matter. I prefer this so I can,

- avoid the mental effort of reassuring myself that the assumptions are good

- boost confidence of the client in the results (looks right = is right).

Once again, your knowledge in this area amazes me. I have only one concern with the results of this study. I have ran many for hours now, is the displacement value. The frame almost seems to 'spin' slightly. I would not expect this and also I have no idea where this is coming from as the frame should be symmetrical. Any ideas?

Once again, your knowledge in this area amazes me. I have only one concern with the results of this study. I have ran many for hours now, is the displacement value. The frame almost seems to 'spin' slightly. I would not expect this and also I have no idea where this is coming from as the frame should be symmetrical. Any ideas?

Your constraints are wrong. you should see deflection more between the corners and not 'at' the corner. And 5+" is quite a bit of deflection unless this thing is 30' across.

What is there to prevent the system from rotation? In a real rigging one can usually spin the load with a finger (or control it with a thin tag line). I used a small rectangular block as a fixture specifically to give us a little 6-axis stability. But still there's not much resistance to spin.

A good FEA solver will prioritize conservation of energy over displacement prediction. As only a little energy is required to get a spin, only a small bit of accumulated error in this solution will equate to a generous spin angle.

Going back to a symmetry model is the clinically correct way to get the assumed symmetric result. I'd cut the model through the middle of two pipes, rather than diagonally between mating plates, to avoid uncertainties about having connectors on the symmetry plane.

A kinematic set of constraints will remove the rotations and will not affect the stress results as they will not introduce any loads to the structure. It would be the preferred way to solve the problem in a static analysis. Further, on loads, it does not affect things greatly whether you use a bearing load or even how you get the load in for this case if your area of concern is not the stresses within say 1 or 2 hole diameters of where the fitting attaches. The contact inclusion adds enormous compute burden for what I would expect to be little change in local stress and no impact outside a couple hole diameters. Bearing allowables tend to be much greater that tear out or shear out or tension failure allowables in a lug. 1/4 symmetry would also impose a kinematic set of constraints. The use of symmetry does have the effect of suppressing non symmetric outcomes but in a static analysis it really has no impact. A static analysis will not give any information on buckling margin in the spreader bars which may be of concern. A non linear large displacement solution would. Margin could be established by increasing the load until it fails to solve (stiffness goes to near zero).

I did it in basically two steps to get a more realistic reaction (I think). Model needs to be "in position" for item lifted - or - you need to assume some CG location of your load.

1) Constrain model at lifted points (i.e. up to sling) and remote load from CG to lifting points (for hooks, links, etc.) Then get your vertical load for each lifting point.

2) For this step I usually just split-plane the holes that will be held by the sling and those holding the load. Here's the tricky part - use 3D sketching to place a point where your slings will end up on the crane, draw a CL from the center of each lifted hole up to this point. You will use that as a constraint direction. Now apply the vertical load to each of your lifting points and using Advanced Fixtures > Reference Geometry, constrain the lifted points along the CL you created. Don't forget to apply gravity if your spreader bar weight something more than zero.

You can show your reaction forces that align neatly with the slings/cables supporting the spreader easily as well.

At the moment there is nothing to prevent rotation, that must be where I am going wrong. I will try this now. Thank you for that, it makes a lot of sense now on how the solvers have behaved in the past.

I see where you are coming from, buckling would definitely be a concern for me, I would also like to know at what point this structure will begin to fail. I would consider the welds joing the tube to the plates the weakest part, do you agree? I have had little experience of non linear studies.

I usually use individual nodes, kitty corner In placement and symmetrical, it might take 3 corners depending on how it's done. You want it stay still but be a le to deflect as it would. The loads on the nodes selected should be near zero.